Cyclone Separator

1. Create Case

After opening SimFlow, we will now create a new case cyclone_separator

1. Go to New panel
2. Provide case name cyclone_separator
3. Click Create Case

2. Import Geometry

After creating case Download Geometry: cyclone.stl

1. Click Import Geometry
2. Select geometry file cyclone.stl
3. Click Open

3. Geometry

After importing geometry, it will appear in the 3D window

1. Click Fit View to zoom out the geometry

4. Scale Geometry (I)

Geometry was created in millimeters, we will scale it to meters

1. Click Options next to the cyclone geometry
2. Select Scale from the options list

5. Scale Geometry (II)

Scale Geometry window will appear on the left side

1. Check Uniform scaling option
2. Set Scaling Factor to 1e-03
3. Click Scale

6. Fit View Geometry

After rescaling geometry, we should zoom in to see the geometry properly

1. Click Fit View to zoom in the geometry

7. Meshing Parameters - Cyclone

Now we will set meshing parameters for cyclone geometry

1. Go to Hex Meshing panel
2. Enable meshing on the cyclone geometry

8. Base Mesh

We will define the base mesh now

1. Go to Base tab
2. Define initial mesh extends

Min [m] -0.1 -0.1 -0.4499
Max [m] 0.1499 0.101 0.5499

(these dimensions have been set, so that inlet, bottom and top faces of the geometry fall slightly outside the box)

3. Define the number of divisions

Division 25 20 100

9. Base Mesh Boundaries

To be able to define different conditions on each boundary of the domain we need to assign an individual name to each side of the base mesh

1, 2. Change the following boundary names accordingly

X+ inlet
Z- bottom
Z+ top

3, 4, 5.Change the following boundary types accordingly

X- wall
Y- wall
Y+ wall
Z- wall

10. Material Point

Make sure the material point is located inside the geometry

1. Go to Point tab
2. Make sure that the material point is set accordingly

Material Point 0 0 0

11. Meshing

Now everything is set up, we can begin the meshing process

1. Go to Mesh tab
2. Click Mesh to start the meshing process

12. Mesh

After meshing process is finished the mesh should appear in the 3D graphics window

13. Setup Solver

We will use MMPICFoam solver. This is a Lagrangian solver based on the Discrete Particle Modelling(DPM) method with Multiphase Particle-in-Cell(MPPIC) collision handling.

1. Go to Setup panel
2. Select Transient filter
3. Select Lagrangian model
4. Pick MMPIC (MMPICFoam) solver
5. Select solver

14. Discrete Phase - Properties

We will now define properties of the discrete phase

1. Go to Discrete Phase panel
2. Set density of the discrete phase

ρ0[kg/m2] 2500

3. Set packing factor

αpacked[-] 0.6

15. Discrete Phase - Injection

We will now define the injection of the discrete phase through the inlet boundary. Mass flow rate of the particles is equal to the mass flow rate of the air that will be defined later in the Boundary Conditions panel.

1. Go to Injection tab
2. Create Boundary Injector
3, 4, 5. Set following parameters accordingly

Total Mass [kg] 1.225
SOI [s] 1
Duration [s] 10
Parcels Per Second 10000

Boundary inlet
U0[m/s] -3 0 0

16. Discrete Phase - Distribution

We will now define a normal distribution of the discrete phase size

1. Go to Distribution tab
2. Set Distribution to Normal
3. Set distribution parameters accordingly

Min [m] 4e-05
Max [m] 3.6e-04
µ [m] 5e-05
σ [m] 2e-04

17. Discrete Phase - Models

We will now define the particle drag model

1. Go to Models tab
2. Select Ergun-Wen-Yu model

18. Discrete Phase - Solution

We will now define methods of computing and interpolating an average of the Lagrangian phase

1. Go to Solution tab
2. Set Averaging method to Dual
3. Expand Source Terms options
4. Set Semi-Implicit discretization of the U term

19. Turbulence

For turbulence modeling, we will use the LES model

1. Go to Turbulence panel
2. Select LES turbulence modeling
3. Select k Equation model

20. Transport Properties - Fluid

Now we will define the transport properties of fluid material

1. Go to Transport Properties panel
2. Click Material Database
3. Select air material
4. Click Apply

21. Solution - PIMPLE

To increase the stability of the simulation we will increase the number of pressure corrector iterations

1. Go to Solution panel
2. Select the PIMPLE tab
3. Increase the number of Correctors to 2

22. Boundary Conditions - Bottom (Particles)

Now we will set a bottom boundary to be transmissive for particles

1. Go to Boundary Conditions panel
2. Select bottom boundary
3. Select Particles tab
4. Change particle interaction to Escape

23. Boundary Conditions - Cyclone (Particles)

1. Select cyclone boundary
2. Set following values accordingly

e [-] 0.97
µ [-] 0.09

24. Boundary Conditions - Inlet (Particles)

We will now set boundary conditions on inlet boundary

1. Select inlet boundary
2. Change boundary condition for inlet to Velocity Inlet
3. Change particle interaction to Rebound

25. Boundary Conditions - Inlet (Flow)

1. Switch to Flow tab
2. Set velocity at inlet

Reference Value [m/s] 20

26. Run - Time Controls

1. Go to Run panel
2. Set Simulation Time [s] to 5
3. Set time step Δt [s] to 1e-04

27. Run - Output

1. Go to Output tab
2. Set Write Control Interval [s] to 0.1 seconds
(it will force solver to write results on the hard drive every 0.1 seconds of the simulation)
3. Click Run Simulation button

28. Run - CPU

This simulation will require high CPU usage and might take several hours to finish the calculation depending on the machine used. To speed up the calculation process increase the number of CPUs basing on your PC capability. We recommend using at least 4 cores for this tutorial. The free version allows you to use only 2 processors in parallel mode. To get the full version, you can use the contact form to Request 30-day Trial

Estimated computation time for 2 processors: 4 hours

1. Switch to CPU tab
2. Use parallel mode
3. Increase the Number of processors
4. Click Run Simulation button

29. Postprocessing - Open ParaView

Open ParaView software to display results

1. Go to Postprocessing panel
2. Start ParaView

30. ParaView - Import Results

After opening the ParaView we will import result from the simulation

1. Click Last Frame to select the latest result set
2. Uncheck lagrangian/kinematicCloud region
3. Click Apply to import results

31. ParaView - Streamlines (I)

We will now plot streamlines

1. Click Stream Tracer button to add streamlines
2. Click Apply

32. ParaView - Streamlines (II)

After creating streamlines we will change the coloring variable to velocity

1. Change the coloring variable to U.bulk

33. ParaView - Import Geometry (I)

In order to display geometry we will load the same case again into ParaView

1. Select Open from menu File menu
2. Select cyclone_separator.foam from file selection window
3. Click OK

34. ParaView - Import Geometry (II)

Now we will select only the outer surfaces

1. Check Mesh Regions
2. Uncheck internalMesh
3. Uncheck lagrangian/kinematicCloud
4. Click Apply

35. ParaView - Clip Geometry

Now we will clip the geometry

1. Select Clip option
2. Select Y Normal
3. Click Apply
4. Select coloring variable of the clip to Solid Color

36. ParaView - Streamtraces

Results are displayed in the graphics window

37. ParaView - Display Particles (I)

In order to display particles you can import the same case into ParaView once again

1. Select Open from the File menu
2. Select cyclone_separator.foam from file selection dialog
3. Click OK

38. ParaView - Display Particles (II)

Now we will select to display particles only

1. Click Mesh regions twice to uncheck all boxes
2. Click Apply

Note that after applying, lagrangian/kinematicCloud will appear on the list of mesh regions. It is checked by default.

39. ParaView - Display Particles (III)

1. Scroll down Properties view
2. Check file format specification
3. Click Apply

40. ParaView - Display Particles (IV)

1. Select particle age as a particle coloring variable
2. Click to adjust scale for selected variable

41. ParaView - Display Particles (V)

We will now disable stream traces and reduce the opacity of the cyclone geometry

1. Click visibility icon next to StreamTracer1 to hide stream traces
2. Select Clip1
3. Adjust geometry Opacity to 0.2

42. ParaView - Results

The results are displayed in the graphics window
This concludes this tutorial.

Note that this tutorial is meant only to demonstrate the capabilities of the software and not to solve the problem in the best possible way. Therefore, some assumptions are taken to keep case setup time and computational time low. In particular, to refine the model, one could in the first place consider refining the grid and choosing a more suitable drag model for the particles (e.g. Ergun-Wen-Yu model). Subsequently, it is worth considering enabling isotropic particle packing, isotropic particle time scale, and stochastic isotropy model.

This website uses cookies to offer you the best experience online. By continuing to use our website, you agree to the use of cookies.